Join Leon van den Heever for an in-depth discussion in this video Extruding the flywheel, part of Modeling a Motorcycle Engine with SOLIDWORKS.
- Continue to use the file you created in the previous video, or feel free to use the lessons file. What we have just done is to create a single sketch with multiple contours. With a sketch selected in the Feature Manager, I'll activate the Extrude Boss/Base command from the Features tab on the command bar to illustrate this better. Since the sketch has multiple contours, SolidWorks automatically activates the selected contour selection box for us within the Boss-Extrude properties. Now if I hover my mouse over the sketch in the graphics view, we can clearly see that we have a top, center, and bottom contour.
The reason we created these multiple contours within a single sketch is so we can use the same sketch on multiple feature commands and can speed up our modeling process. Use this technique as often as it permits within your design intent, but be careful not to try and cram the entire design into one or only a few sketches since this could be more of a hindrance when needing to make changes down the line. A good modeler will be flexible and combine the multiple strategies SolidWorks offers us.
Select the circle contour. If you do have multiple selections in these property selection boxes, you can right-click an entry and delete it, or right-click and clear all selections. Make sure that you only have the circle contour selected. We will be extruding in two directions with different extrude depths in this feature. For that reason, set Direction One's depth to one millimeter. Activate the Direction Two's options by selecting this box, and set the second direction's depth to 40 millimeters.
Enter, and enter again to complete the command. We know have our first Boss-Extrude in the Feature Manager. Clicking on the plus icon to the left of the extruded feature icon, expand the feature, and again select Sketch One so we can reuse it for our next feature as well. Do another Extrude Boss/Base, and this time select both the top and bottom arc contours in the graphics view. We will extrude both contours in the same feature since their extrusion depths will be identical.
Note that you do not have to hold the control key when using properties multiple selection boxes. Simply click on what you want to include. For this time we will only be extruding in one direction so we only need to set Direction One's properties. First reverse the extrude direction by clicking on this icon with the two arrows. For our design intent, we want the depth of these contours to be the same depth as Direction Two of the circle extrude. Furthermore, if the extrude depth had to be changed, we want to ensure that this extrusion's depth will automatically update to the same depth.
To achieve this, let's select the Up to Surface End Condition from the End Condition drop-down box. With the Up to Surface End Condition selected, the properties have now changed, and SolidWorks is now asking us to select a plane or face. In the graphics view, position your mouse cursor over the cylindrical face of the circle extruded. Right mouse click and activate the Select Other command from the right mouse options. Using this tool gives us the ability to select faces located behind other faces easily without having to rotate our graphics view which is very handy.
From the pop-up dialog, select the face, or alternatively, select the face directly in the graphics view. Complete the extrude command by clicking on one of the green okay icons. Note that if I did not move my mouse, the cursor feedback indicates that I can do a right-click of the mouse to complete the command as well. Again, very efficient. Control-S to save your work, and I'll see you in the next video.
Need a better background in SOLIDWORKS before you can continue? Check out SOLIDWORKS 2014 Essential Training.
- Sketching the flywheel
- Building and cutting the flywheel shafts
- Filleting the flywheels
- Splitting the connecting rod
- Building the sprocket
- Modeling the camshaft
- Combining parts into an assembly